Announcements
Attention for Customers without Multi-Factor Authentication or Single Sign-On - OTP Verification rolls out April 2025. Read all about it here.

CAM Post Does Not Reset G43 For a Repeat Tool

tomGKJVK
Advocate

CAM Post Does Not Reset G43 For a Repeat Tool

tomGKJVK
Advocate
Advocate

I just noticed this problem a couple weeks ago.  When I'm using the same tool twice in a row for different operations, it does not set G43 the second/third/etc times.   I'm using G28 and M01 at the end of each operation, which is clearing the tool offset.   So, it needs to put G43 at the beginning of the next op even though it's the same tool.  Safe Start All Operations is checked.

 

I'm using the Haas (pre-ngc) Post.   

0 Likes
Reply
Accepted solutions (1)
670 Views
4 Replies
Replies (4)

engineguy
Mentor
Mentor

Unless there is a G49 command somewhere in the code which is the command that will cancel a G43/G44 Tool Length Offset or something specific to the HAAS control that would cancel the G43/G44 then that is what I would consider normal, if there has not been a change to a different tool in between the operations using the same tool then the G43 offset "stands" until it is cancelled either by a change to a different tool or a G49 command is posted.

 

Nothing to worry about IMHO, hope that helps Smiley Happy Smiley Happy

 

Regards

Rob

0 Likes

tomGKJVK
Advocate
Advocate
Thanks for the reply. This however is not the case. Tool length compensation is being cleared between operations with the same tool and the subsequent operations with the same tool are being executed at Machine zero instead of tool zero. There’s no G49 in the code.

G28 automatically suspends the tool length compensation.

I can use G53 in most cases instead, but this is still a glitch with the post that should be corrected. Tool length compensation must be reinstated after a G28.


0 Likes

engineguy
Mentor
Mentor
Accepted solution

@tomGKJVK

 

OK, yes, it appears that in the HAAS controls the G28 does indeed cancel the tool height offset as you describe.

 

However I have tried a simple 2D pocket using the same tool for the roughing out and the finish contour, I have selected the optional stop M01, Use G28 instead of G53 and used the Safe Start and the Post Processor is outputting the code shown below which as I read it is correct, the G28 line is there, (N1675) the M1 line is there (N1685) and the safe start / are there (N1675, 1690 and 1705) and below all that there is a new G43 H* line (N1720) as required so I am thinking that you may have an older version of the Pre-NGC Post Processor, have you tried going to the library and downloading the latest Pre-NGC post here https://cam.autodesk.com/hsmposts?

 

Here is the code as generated here by the Pre-NGC PP that I have, last modified 40 days ago :-

N1645 X-25.397 Y22.219 Z-9.759
N1650 X-25.373 Y22.134 Z-9.67
N1655 X-25.353 Y22.081 Z-9.559
N1660 X-25.329 Y22.029 Z-9.447
N1665 X-25.31 Y21.995 Z-9.2
N1670 G0 Z10.

(2D Contour)
N1675 / G28 G91 Z0.
N1680 G90
N1685 M1
N1690 / T1 M6
N1695 S4000 M3
N1700 G54
N1705 / M8
N1710 G0 Z15.
N1715 G0 X23.6 Y-0.8
N1720 G43 H1
N1725 G0 Z5.

 

The little test program I did is attached

Regards

Rob

 

P.S. Sorry, forgot to say I did it in Metric, I default to that Smiley Happy  Smiley Happy  Smiley Happy

 

0 Likes

tomGKJVK
Advocate
Advocate
Yes! I was on an old post. Thank you, that fixed it.
0 Likes